Fanuc Series 15i/150i-MA (Programming) Operators Manual

17.CUSTOM MACRO PROGRAMMING B-63324EN/03
- 636 -
Sample program
The same operation as the drilling canned cycle G81 is created using a
custom macro and the machining program makes a modal macro call.
For program simplicity,all drilling data is specified using absolute
values.
- Calling format
G66 P9110 Zz Rr Ff Ll ;
Z : Coordinates of position Z (absolute specification only)........(#26)
R : Coordinates of position R (absolute specification only) .......(#18)
F : Cutting feedrate .......................................................................(#9)
L : Repetition count
- Program that calls a macro program
O0001;
G28 G91 X0 Y0 Z0;
G92 X0 Y0 Z50.0;
G00 G90 X100.0 Y50.0;
G66 P9110 Z-20.0 R5.0 F500;
G90 X20.0 Y20.0;
X50.0;
Y50.0;
X70.0 Y80.0;
G67;
M30;
Operation 1
Operation 3
Operation 2
Position I
Position R
Z=0
Position Z
Operation 4
The canned cycle consists of the
following basic operations:
Operation 1 : Positioning along the X-
axis and Y-axis
Operation 2 : Rapid traverse to point R
Operation 3 : Cutting feed to point Z
Operation 4 : Rapid traverse to point R
or I
R
Z
Rapid traverse
Cutting feed

Leave a Reply

Your email address will not be published. Required fields are marked *